Please Test My Stick Fonts and Let Me Know If They Work For You

[lloydsp]

Ahh... TOOLPATHS!

You did not say, "cuts on the mill."

You know that when you generate toolpaths, ALL the paths the tool will take, including lifts up to the safe clearance height, recursions necessary to begin a new cut, and all sorts of apparently "unnecessary" tool motions will be shown -- not JUST the actual cuts, themselves.

You may just be looking at EVERY motion the tool will make, and confusing many of those for actual cuts.

Have you run this through CutViewer, or some other simulator, to see what the work will look like when finished?

(HINT... change the machining colors to something drastically bright for actuall cuts, and dim, dull colors for everything else, then look at the toolpaths, and see what you see.)

LLoyd

[CanAm1]

LLoyd,
Unfortunately I have 4 or 5 cut already trying to get things to work.
I am going to try and attach some screen shots of what I am getting.

First shot is of the file in cambam... Look OK.
Second is a shot of the tool paths..
Third and forth show mach3 shots of how it will look. I panned the image to show how the letters are goofed up.
I'll post an actual cutting in a second...

Mark

[CanAm1]

All,

And last but not least is one of my actual engravings.
You can see how the letter "I" in the word size is capital, but in cambam it's small case which I want.
Also you can see how the 2 small case "U"s in up and cut have there tops filled in..

Thanks

Mark

[Hans_G]

What is your clearance plane set to?  Does the bit sufficiently clear the stock for rapids?  The examples of the mis-cuts seem like the cutting tool might not be clearing the stock during rapids???

[blowlamp]

Mark.
Try setting the MaxCrossoverDistance to zero in the Engrave 1 MOP and see if it changes anything. I think the distance between the body of the lowercase 'i' and it's 'dot', is less than than the 0.7 MaxCrossoverDistance of the ToolDiameter, that you are using for the cut and I think the same thing applies to the lowercase 'u' too.

Martin.

[GeorgeRace]

What really seems strange is that the "i" in Mill is OK, but the "i" in Size is not.   And they are close together in the same row.  Could it have something to do with the IJ setting in Mach3 or CamBam?
George

[lloydsp]

What really seems strange is that the "i" in Mill is OK, but the "i" in Size is not.   And they are close together in the same row.  Could it have something to do with the IJ setting in Mach3 or CamBam?
George

George, note that the toolpaths are different on the two 'i's, and that both legs of the U are cut down in the same direction, forcing the tool to do a "jump".

I'm guessing that the basic tool diameter is large, and the crossover distance is too large.  Those bad cuts are obviously NOT full-depth engraving (especially, look at the offset in the top of the bad 'i', and the 'u').  It looks to me almost as if the tool began moving up to safe, but started the rapid before getting up to the clearance height.

That, then, would be a setup issue -- either the crossover distance is too large, or Mach3 is somehow misbehaving on very small details where the tool must move only a few thousanths between moving up to clearance and down to the target depth again.

LLoyd

[CanAm1]

  Success 

First off, my clearance plane was set at 1/8 inch (pretty high) so I was not dragging the bit.
It was the MaxCrossoverDistance setting that did the trick.. Set it at zero, re-ran the tool path and g code generation and you could tell right away in mach3 that things were better. Of course I had to run an engrave to test things out and it turned out right on the money. Cool...
Since I am still going to consider myself a fledgling beginner.. What and how (in simple terms) does this MaxCrossoverDistance setting work? Also, should or can I keep this setting at zero for everything I do? (That way I don't have to worry about it)
Thanks so much guys... It's great when problems are solved...

Mark

[dh42]

Hello

Little info about MaxCrossOver here

http://www.cambam.co.uk/forum/index.php?topic=1551.msg8631#msg8631

You can set it to 0 for engraving, but not for other MOP, because you will get round trip in Z at each change of toolpath (in a pocket by example)

++
David

[GeorgeRace]

Glad you got it working Mark, and thanks for letting us know what the problem was.
George

[blowlamp]

The MaxCrossoverDistance is provided to reduce the number of Z axis retracts when moving from one toolpath to another and the value entered represents the decimal fraction of the selected ToolDiameter for that MOP.

So with the MaxCrossoverDistance set to 0.7, this means that a 10mm diameter tool can move up to 7mm in the X,Y plane, without retracting between cuts, provided that the straight line distance from the end of one toolpath to the beginning of another is less than 7mm, but a 5mm diameter tool would only move up to 3.5mm, with the same setting.

If you leave MaxCrossoverDistance set to zero, then you will see more tool retracts.

The upshot is that if you change your ToolDiameter or text size, then the retract behaviour changes as well.


Martin.

[CanAm1]

Hello All,

Appreciate all the help once again.

I think I have a slightly better grasp of what MaxCrossoverDistance does.

I thought I would close with a shot of the finished plaque with all its lettering correct.

Mark

[lloydsp]

Mark, I hate to say it, but you have still got a problem on that placard.

This time, it's a typo, not a milling error.
(duhhhoooo!  I HATE it when that happens!)

LLoyd

[CanAm1]

Oh C*#p.....

Your right LLoyd.

Oh well, I guess the old saying, "practice makes perfect" comes to mind.

I should have slowed down once things started working right.

Something to tinker with tonight...

Mark

[twocik]

I've tried everything to get the tool path to just make a single line (stick font), didn't realize it would be this hard.  Any pointers ?